I am contemplating the most efficient ways to fix problems either mid operations or after completion. A common occurrence in almost all of my builds. It is taking hours to edit tool paths on large projects with all the rest chains, it gets very time consuming up to half a day to make any adjustments.
Was hoping I could start a discussion to get some advice or tips.
Simulate and save file at point of repair needed, use new setup, enable rest machining and load from file.
Repair model in design, ignore outdated tool paths in manufacture and use rest machining from last operation even though it is outdated leaving a mess with your tool paths.
Copy part and paste, make repair with design, make new setup in manufacture with new part only recognized.
Do not use rest machining, set depth to level of repair needed let tool paths think you are going deeper then you really are.
After completion rebuild entire tool path structure for next run.
Could someone help me with any tips on how to relocate stock accurately for precise machining? My best efforts at precision re calibrating with the touch probe after re homing are always off. If I do not keep it on the same homing operation in the same location I can forget about any matching edges.
In such situations, I have used rest machining toolpaths to fix things (most common scenario: shave off an extra 0.01" of material around a given perimeter/pocket/wall) but the toolpath list can indeed get pretty messy. I don’t mind because I mainly do one-off parts, but if I were doing any kind of production, I would certainly take the time recreate the minimal amount of toolpaths based on the final design.
One trick that could be of interest to you, is that you can use any object as the definition of your stock (by selecting “Mode = From Solid” in the Stock/setup menu). So say you have cut v1 of your part, then realize you want to cut an additional feature in it somewhere. You could : create a new setup where the stock IS your v1 part, then proceed to modify things for a v2 and create new toolpaths in that setup : the new toolpaths will be computed based on that specific stock, so they will only try to remove material that was not already removed to cut v1. It’s equivalent to rest machining, but you don’t have to maintain a huge chain of toolpaths that do rest machining on top of each other (which indeed can take ages to recompute)
For precise relocation of stock you may want to consider cutting a custom jig for your piece ? The simplest version of that is cutting a pocket in some piece of MDF, that has the same outline as your stock/intermediate piece. You can zero anywhere, cut that jig pocket, insert your piece, and since you will be managing both the jig pocket and the actual piece in the same model in Fusion, you can reference all toolpaths from that same zero.
If you do have to adjust zero, and at the risk of stating the obvious, you don’t have to redo XYZ, you can just e.g. adjust Z zero alone. Typical case: the location where you set X0Y0Z0 initially has been cut away, and you just need to readjust Z0: you can jog to some other part of the piece where the Z0 plane still exists, and re-zero Z (only) there, without having modified X or Y.
Side note: do you have the mechanical limit switches ? If so and if you are looking for increased re-homing repeatability/accuracy, you can upgrade to proximity sensors instead.
Hi Julien,
I had not worked with the from solid option yet. Thank you very much for the valuable information. I will practice with these methods you have mentioned.
My limit switches are the stock 3 XXL as of 2 months ago. Do you have a link for the proximity setup?
Here’s a setup that I use, because I have to cut off the corner of the part that was my zero point. In Vcarve, there’s an item in the material setup where you can specify an XY instead of just the center or lower left corner. I choose the offset between my jig and where the origin is set in my part’s design. (The offset can judiciously be chosen when one engineers the jig and part.)
The jig becomes part of the part and should always be labeled to match the part.
Very nice Tex, I should mention that my Z problems are a thing of the past with the bit setter. It has really helped me very much.
Re-finding X Y after removing and re attaching a part is where I fail every time. If you remove the jig and re attach it, and try to re carve on a previous piece.
As far as I know, Carbide 3D does not sell them (yet…Luke used to sell them on his beaver cnc site), but people have discussed alternate sources in various threads for example this one.
Note that I’m not specifcally advocating for upgrading to proximity switches, just reporting that they exist and that people seem to find them more accurate/repeatable (I vaguely remember some threads where values/measurements have been discussed).
I can see where that could be a problem depending on how close you need to be to the original. I’ve actually done that in my normal workflow, but have designed the part to allow for misalignment. However, I’m not trying to recut small text or fit into previously cut fine detail. That would be a bit scary.
EDIT: Just to add a bit more detail, when I cut the jig’s profile for the part, I use the same vector used to make the part but add an allowance in the toolpath of 0.010". That allowance works for most of my parts, but I can see where it could be made tighter than that.
I have had in my very limited experience what seems like some really impressive results with the Shapeoko. Taking things down to 0 and having them fit together perfectly. Was able to reproduce with a flip jig as well.
